Sketch constrain to line piercing through a plane

[Anonymous]

Hello all

Solidworks has a function in which you can constrain a sketch to a line piecing through the sketch plane at an angle. For example, if I wanted to add a gusset between two right angle plates, with the gusset at a 45 degree angle. I can add a 45 degree sketch plane and sketch the gusset. Can I get the ends of the gusset sketch to constrain to the plate edges where they pierce through the gusset sketch plane.

There is a screenshot attached.

Regards

Andrew

[jhackney1972]

You were not very clear how the 45 degree plane was oriented to the two 90 plates and your PDF was not clear either.  I did a screencast using two different planes containing two piercing sketch lines and showed how they are terminated by the Rib command at the faces of the plates.  I have included the part file in Inventor 2018 format.

[Anonymous]

I have attached another image of the weldment and you can see the t-section brace attaching to the UC. The flange is drawn on a plane at 60° to the ground plane. If I can constrain sketch points where the UC plane/edge intersects the sketch plane, I can easily size the flange correctly, and visa versa at the floor plate.

Regards

[SBix26]

It will be much easier for us to offer assistance if you attach an actual example file, and if you insert images in the text of your message instead of attaching them (use the Photos tool).

If I'm understanding correctly, one way to accomplish this is to create a work point at the axis/plane intersection, then project that to the sketch.  I don't believe this is possible from within the sketch, but if you attach an example we don't have to guess or try to create our own example.  What version of Inventor did you say you're using?

Sam B
Inventor Pro 2018.2.3 | Windows 7 SP1
LinkedIn

[Anonymous]

Hi Sam

Yes that does it. Though I cannot move the point up the model tree and above my sketch, in order to project it in the sketch. If I did it when creating the work plane (for the sketch) it would work.

[Anonymous]

Thanks Sam, I cannot attach a model, but will post photos in the text next time.

Andrew

[SBix26]

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@Anonymous wrote:

Hi Sam

Yes that does it. Though I cannot move the point up the model tree and above my sketch, in order to project it in the sketch. If I did it when creating the work plane (for the sketch) it would work.

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Sure you can-- pull the EOP (End of Part) from the bottom of the browser to just above your sketch, create the new workpoint, then pull the EOP back down.  Or, create the workpoint, then drag it in the browser to just above the sketch.

Sam B
Inventor Pro 2018.2.3 | Windows 7 SP1
LinkedIn

[Anonymous]

I'm in an assembly using in-place/in-context parts for the plate elements so there is no EOP marker. For some reason, even if I don't reference anything at or below my sketch part, I cannot drag it above the sketch part.

[SBix26]

Sorry, I'm having trouble visualizing from what you've attached so far.  Are you creating your sketch in a part or in an assembly?

Sam B
Inventor Pro 2018.2.3 | Windows 7 SP1
LinkedIn

[Anonymous]

The sketch is in a part. The part has been placed in context into an assembly. The part sketch (for the t-piece flange) needs to reference other part edges, as well as other work planes. In SW for example, when I'm in the sketch generating the gusset flange part, I can constrain the sketch to other part edges that pierce through the sketch plane. It doesn't look like inventor has anything like this feature. As you have pointed out, I could use a work point with a bit of prior messing around.

[SBix26]

Ah, yes.  I wasn't thinking about adaptive modeling, which I avoid like the plague.  This is the sort of design in which I'd use top-down modeling techniques such as multi-solid master models, master sketches, etc.  Similar to Frame Generator, which I see you've used in this assembly.

Sam B
Inventor Pro 2019.0.0 | Windows 7 SP1
LinkedIn

[Anonymous]

Hi Sam

Yes what you suggest is certainly more robust, but adaptive modeling is so fast. It is disappointing that it can be a pain in the neck and that most people seem to avoid it. I used it a lot in SW where it seems to be more functional and less prone to dramas. I have found that it is useful for rapid layouts, then the adaptivity can be removed and links broken to avoid problems, and the parts built up from there. The inability to constrain sketches to out of plane lines is a significant drawback when building adaptive assemblies I must say.

Thanks for your input.

Andrew